Forums

What is the maximum signal frequency SPICE can handle ?

Started by Unknown March 22, 2012
Could some electronics guru tell me what 
is the maximum signal frequency that the 
SPICE can handle ? I have experimented 
with a simple low pass LC filter and found 
that the maximum input frequency that it
can handle (before the output looks like
junk) is 1 THz (10^12 Hz) even when the 
cutoff has been set to 150 THz. What are
your experiences with this ?
    
On 2012-03-22, dakupoto@gmail.com <dakupoto@gmail.com> wrote:
> Could some electronics guru tell me what > is the maximum signal frequency that the > SPICE can handle ?
blue perhaps. how good are your parts models? -- &#9858;&#9859; 100% natural
On 2012-03-22, dakupoto@gmail.com <dakupoto@gmail.com> wrote:
> Could some electronics guru tell me what > is the maximum signal frequency that the > SPICE can handle ?
That depends on how low you can set the step size and how well your models match real parts. There's a theoretical limit where you run out of mantissa in the floating point but you'd be simulating gamma ray frequencies before you hit that limit. I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what appeared to be consistent results. At the end of the day it's just arithmentic. -- &#9858;&#9859; 100% natural
On Mar 22, 5:30=C2=A0am, Jasen Betts <ja...@xnet.co.nz> wrote:
> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote: > > > Could some electronics guru tell me what > > is the maximum signal frequency that the > > SPICE can handle ? > > That depends on how low you can set the step size and how well your > models match real parts. > > There's a theoretical limit where you run out of mantissa in the > floating point but you'd be simulating gamma ray frequencies before > you hit that limit. > > I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what > appeared to be consistent results. > > At the end of the day it's just arithmentic. > > -- > =E2=9A=82=E2=9A=83 100% natural
YES! separate math limit from simulation effectiveness limit. IME, for discrete components at around 10MHz, PSpice seems to no longer represent reality. I've always attributed that to the 'weakness' in the modeling, but never bothered to pursue further. Inside components, translate that to SMALL geometry, at around 100MHz. Mathematically I constantly use to beyond 1GHz, however, more for 'learning' what's going on than 'describing' what's going on. At 1+ THz, EVERYTHING must be acting like a radiating, transmission line. Can't imagine the complexity of a useful model. Even the wavefronts through conduction must have some effects, right? Be like trying to model the acoustics of a concert hall with all that wave/ reflections, etc.
Robert Macy wrote:
> > On Mar 22, 5:30&#2013265922; am, Jasen Betts <ja...@xnet.co.nz> wrote: > > On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote: > > > > > Could some electronics guru tell me what > > > is the maximum signal frequency that the > > > SPICE can handle ? > > > > That depends on how low you can set the step size and how well your > > models match real parts. > > > > There's a theoretical limit where you run out of mantissa in the > > floating point but you'd be simulating gamma ray frequencies before > > you hit that limit. > > > > I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what > > appeared to be consistent results. > > > > At the end of the day it's just arithmentic. > > > > -- > > &#9858;&#9859; 100% natural > > YES! separate math limit from simulation effectiveness limit. > > IME, for discrete components at around 10MHz, PSpice seems to no > longer represent reality. I've always attributed that to the > 'weakness' in the modeling, but never bothered to pursue further. > Inside components, translate that to SMALL geometry, at around 100MHz. > > Mathematically I constantly use to beyond 1GHz, however, more for > 'learning' what's going on than 'describing' what's going on. > > At 1+ THz, EVERYTHING must be acting like a radiating, transmission > line. Can't imagine the complexity of a useful model. Even the > wavefronts through conduction must have some effects, right? Be like > trying to model the acoustics of a concert hall with all that wave/ > reflections, etc.
Below about 10 THz, the method of moments (MOM) works okay. Above there, material dispersion and limited conductivity make full-wave simulations de rigueur--FEM or FDTD, usually. The conductivity limit comes in because the effective dielectric constant of a normal conductor is epsilon = epsilon.re + j sigma/omega so conductors look steadily less conductive as the frequency goes up. Antenna simulations using MOM at 28 THz (CO2 laser territory) look vaguely like the fullwave ones, and vaguely like the experiments, but if you go any higher, all resemblance is lost. My 200 THz stuff was all fullwave. Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 845-480-2058 hobbs at electrooptical dot net http://electrooptical.net
On Mar 22, 7:50=C2=A0pm, Phil Hobbs
<pcdhSpamMeSensel...@electrooptical.net> wrote:
> Robert Macy wrote: > > > On Mar 22, 5:30=C3=82 am, Jasen Betts <ja...@xnet.co.nz> wrote: > > > On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote: > > > > > Could some electronics guru tell me what > > > > is the maximum signal frequency that the > > > > SPICE can handle ? > > > > That depends on how low you can set the step size and how well your > > > models match real parts. > > > > There's a theoretical limit where you run out of mantissa in the > > > floating point but you'd be simulating gamma ray frequencies before > > > you hit that limit. > > > > I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave wh=
at
> > > appeared to be consistent results. > > > > At the end of the day it's just arithmentic. > > > > -- > > > =C3=A2=C5=A1=E2=80=9A=C3=A2=C5=A1=C6=92 100% natural > > > YES! separate math limit from simulation effectiveness limit. > > > IME, for discrete components at around 10MHz, PSpice seems to no > > longer represent reality. =C2=A0I've always attributed that to the > > 'weakness' in the modeling, but never bothered to pursue further. > > Inside components, translate that to SMALL geometry, at around 100MHz. > > > Mathematically I constantly use to beyond 1GHz, however, more for > > 'learning' what's going on than 'describing' what's going on. > > > At 1+ THz, EVERYTHING must be acting like a radiating, transmission > > line. Can't imagine the complexity of a useful model. Even the > > wavefronts through conduction must have some effects, right? Be like > > trying to model the acoustics of a concert hall with all that wave/ > > reflections, etc. > > Below about 10 THz, the method of moments (MOM) works okay. =C2=A0Above > there, material dispersion and limited conductivity make full-wave > simulations de rigueur--FEM or FDTD, usually. > > The conductivity limit comes in because the effective dielectric > constant of a normal conductor is > > epsilon =3D epsilon.re + j sigma/omega > > so conductors look steadily less conductive as the frequency goes up. > Antenna simulations using MOM at 28 THz (CO2 laser territory) look > vaguely like the fullwave ones, and vaguely like the experiments, but if > you go any higher, all resemblance is lost. =C2=A0My 200 THz stuff was al=
l
> fullwave. > > Cheers > > Phil Hobbs > > -- > Dr Philip C D Hobbs > Principal Consultant > ElectroOptical Innovations LLC > Optics, Electro-optics, Photonics, Analog Electronics > > 160 North State Road #203 > Briarcliff Manor NY 10510 > 845-480-2058 > > hobbs at electrooptical dot nethttp://electrooptical.net
spice small documentary www.commitmentiseverything.com/monkeyman.html?utm_source=3D554261 www.commitmentiseverything.com/moochwala.html?utm_source=3D554261
On Thu, 22 Mar 2012 07:31:12 -0700 (PDT), Robert Macy
<robert.a.macy@gmail.com> wrote:

>On Mar 22, 5:30&#2013266080;am, Jasen Betts <ja...@xnet.co.nz> wrote: >> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote: >> >> > Could some electronics guru tell me what >> > is the maximum signal frequency that the >> > SPICE can handle ? >> >> That depends on how low you can set the step size and how well your >> models match real parts. >> >> There's a theoretical limit where you run out of mantissa in the >> floating point but you'd be simulating gamma ray frequencies before >> you hit that limit. >> >> I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what >> appeared to be consistent results. >> >> At the end of the day it's just arithmentic. >> >> -- >> ?? 100% natural > >YES! separate math limit from simulation effectiveness limit. > >IME, for discrete components at around 10MHz, PSpice seems to no >longer represent reality.
I have used PSpice to model RF stages at 5GHZ, no problem. If you don't set a "Maximum Time-step" small enough (my rule-of-thumb is 1/32 of the period of the highest frequency... or smaller), you will get a jagged sampling output.
>I've always attributed that to the >'weakness' in the modeling, but never bothered to pursue further.
That might be with behaviorally-modeled devices.
>Inside components, translate that to SMALL geometry, at around 100MHz. > >Mathematically I constantly use to beyond 1GHz, however, more for >'learning' what's going on than 'describing' what's going on. > >At 1+ THz, EVERYTHING must be acting like a radiating, transmission >line. Can't imagine the complexity of a useful model. Even the >wavefronts through conduction must have some effects, right? Be like >trying to model the acoustics of a concert hall with all that wave/ >reflections, etc. >
Finite element analysis? ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Wed, 21 Mar 2012 23:23:24 -0700 (PDT), dakupoto@gmail.com wrote:

>Could some electronics guru tell me what >is the maximum signal frequency that the >SPICE can handle ? I have experimented >with a simple low pass LC filter and found >that the maximum input frequency that it >can handle (before the output looks like >junk) is 1 THz (10^12 Hz) even when the >cutoff has been set to 150 THz. What are >your experiences with this ? >
There should be lots of floating-point range to get to THz. There are a few Spice parameters that might matter. Minimum time step is one. LT Spice has "chgtol" and "cshunt" and "cshuntintern" that will matter at super speeds, possibly others. There is a "minimum inductance damping" thing, too. The default Spice is probably optimized/compromised for speed and convergence with practical circuit values and speeds. After all, you can't really make a 150 THz LC filter. -- John Larkin, President Highland Technology, Inc jlarkin at highlandtechnology dot com http://www.highlandtechnology.com Precision electronic instrumentation Picosecond-resolution Digital Delay and Pulse generators Custom laser controllers Photonics and fiberoptic TTL data links VME thermocouple, LVDT, synchro acquisition and simulation
On 22 Mar., 16:47, Jim Thompson <To-Email-Use-The-Envelope-I...@On-My-
Web-Site.com> wrote:
> On Thu, 22 Mar 2012 07:31:12 -0700 (PDT), Robert Macy > > > > > > > > > > <robert.a.m...@gmail.com> wrote: > >On Mar 22, 5:30=A0am, Jasen Betts <ja...@xnet.co.nz> wrote: > >> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote: > > >> > Could some electronics guru tell me what > >> > is the maximum signal frequency that the > >> > SPICE can handle ? > > >> That depends on how low you can set the step size and how well your > >> models match real parts. > > >> There's a theoretical limit where you run out of mantissa in the > >> floating point but you'd be simulating gamma ray frequencies before > >> you hit that limit. > > >> I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave wha=
t
> >> appeared to be consistent results. > > >> At the end of the day it's just arithmentic. > > >> -- > >> ?? 100% natural > > >YES! separate math limit from simulation effectiveness limit. > > >IME, for discrete components at around 10MHz, PSpice seems to no > >longer represent reality. > > I have used PSpice to model RF stages at 5GHZ, no problem. =A0If you > don't set a "Maximum Time-step" small enough (my rule-of-thumb is 1/32 > of the period of the highest frequency... or smaller), you will get a > jagged sampling output. >
all spice knows is time steps and equations it doesn't really know the physical concept of frequency -Lasse